I am trying to make a custom footprint that has 2 custom-shape pads that need to be covered with the soldermask. I.e., these 2 pads will not have any exposed copper. After countless attempts and forum searching I can't seem to get it to work.
In the pattern editor, I have tried right clicking on the pad and clicking Mask/Paste settings, then changing top solder mask, bottom solder mask. In all of the other forum posts everybody is saying there is an option for none or something similar, but the only options I see are Common State, Open, and Tented. None of these 3 options create a covered pad. I have also tried adding filled shapes of top mask just to be sure that I am understanding the function properly, but the top-mask shape is more of an ant-mask (i.e., it creates an opening in the top mask).
The only option I can think of is to convert the pads to shapes, and place a tiny pad in the corner of the pseudo-pad shape. I have gotten this to work, but like I said, I would prefer to have no copper exposed.
Does anybody have any suggestions?
Custom Footprint Covered Pads in Version 3.3.1.3
Re: Custom Footprint Covered Pads in Version 3.3.1.3
Select the pads you want the solder mask to cover and make them "tented", change the solder paste to none, save the part. Open PCB editor, place the part, export Gerber, top only, preview, you should not see the pads that were tented which means the pads are covered with the solder mask.
Re: Custom Footprint Covered Pads in Version 3.3.1.3
Okay, so I guess the limitation I was missing was that this has to be done in the PCB Editor tool, not in the Footprint Editor tool. It seems that no matter what settings I choose in the Footprint Editor, there is no effect. But in the PCB editor, I can select each pad and use the settings you describe and it works like a charm.
Thanks!
Thanks!
Re: Custom Footprint Covered Pads in Version 3.3.1.3
The pattern editor can make the mask changes, when you use the pattern in a component then place it on the PCB the mask setting will be as set in the pattern editor. If it is something that will always be tented use the pattern editor, for one-of parts use the PCB editor. You can view the results of the mask setting in the PCB editor...a18rhodes wrote: ↑16 May 2019, 12:48 Okay, so I guess the limitation I was missing was that this has to be done in the PCB Editor tool, not in the Footprint Editor tool. It seems that no matter what settings I choose in the Footprint Editor, there is no effect. But in the PCB editor, I can select each pad and use the settings you describe and it works like a charm.
Thanks!
Re: Custom Footprint Covered Pads in Version 3.3.1.3
Interesting, it seems when do this in the pattern editor instead of the PCB editor, the pads end up still being exposed in the preview.
Re: Custom Footprint Covered Pads in Version 3.3.1.3
Now we get to the tricky part: When you updated a pattern you must delete it from the component in the component editor and replace it with the updated pattern, update the component in the schematic THEN replace the component on the PCB with the updated component as in update PCB from schematic. One day I can only hope for a sync function across the product.
A problem I run into is making changes to a pattern in PCB and later updating the PCB from the schematic which overwrites the changes I did to the pattern in PCB editor.
Re: Custom Footprint Covered Pads in Version 3.3.1.3
I am having this issue. Or similar, anyway.
I have a part where I want to have solder mask over *part* of a rectangular pad. I want the middle covered, and the two ends open and solder-pasted.
In the Pattern Editor I drew a square over the covered part of the pad, and made it top mask type. I can see it, but it is layered underneath the copper pad, and when I preview it in PCB Layout (after doing all the library saving and updating you mentioned), the pad in not covered.
I'll attach a screenshot of my part.
Any ideas on how to make this work?
Thank you!
I have a part where I want to have solder mask over *part* of a rectangular pad. I want the middle covered, and the two ends open and solder-pasted.
In the Pattern Editor I drew a square over the covered part of the pad, and made it top mask type. I can see it, but it is layered underneath the copper pad, and when I preview it in PCB Layout (after doing all the library saving and updating you mentioned), the pad in not covered.
I'll attach a screenshot of my part.
Any ideas on how to make this work?
Thank you!
- Attachments
-
- Mask_Shape.png (4.07 KiB) Viewed 621 times
-
- Posts: 7
- Joined: 12 Apr 2019, 12:07
Re: Custom Footprint Covered Pads in Version 3.3.1.3
Gerber data, and in this case diptrace, shows the mask layer as a negative, meaning if it shows up in the layer the board house is to NOT apply mask there. So when you draw the square over the center diptrace thinks you intend to have it as an opening in the masking, not additional masking.
To get the effect you are looking for right click on the pad and set both top and bottom mask to tented. This means there will not be any opening in the mask layer for the pad at all. Now draw the squares where you do want an opening. Below are images of a quick demo of the same kind of part you are working with to help show how it treats the mask layer. The top 2 locations have the pad set to tented, you can do this by right clicking the pad and going to mask/solder settings.
Once nice thing to note is this can be done in the pattern editor so you don't have to worry about only being able to make it work in the pcb editor
Hope this helps
To get the effect you are looking for right click on the pad and set both top and bottom mask to tented. This means there will not be any opening in the mask layer for the pad at all. Now draw the squares where you do want an opening. Below are images of a quick demo of the same kind of part you are working with to help show how it treats the mask layer. The top 2 locations have the pad set to tented, you can do this by right clicking the pad and going to mask/solder settings.
Once nice thing to note is this can be done in the pattern editor so you don't have to worry about only being able to make it work in the pcb editor
Hope this helps
Re: Custom Footprint Covered Pads in Version 3.3.1.3
Yes, thanks! After I posted my question, I kept playing with it, and that's what I came up with, also. (I would have posted an update, but they hadn't approved my first post yet). The trick is to not only think in the negative, but to tent the pad, too.